How does the Inlay Toolpath work in VCarve Pro & Aspire for straight, stepped, and V-Carve inlays?

Overview

The Inlay toolpath calculates profile or pocketing toolpaths with automatic compensation for the tool radius, so the cut-out male plug and the female pocket or hole fit together. Without this compensation, the rounded interior corners of the pocket would prevent sharp-cornered male parts from seating, and the rounded outside corners of a cut-out part would not match the pocket. The inlay toolpath rounds both parts to match. It is available in both VCarve Pro and Aspire.

Critical rule: The same tool must be used for both the male (plug) and female (pocket/hole) parts of an inlay. Different tools mean the parts won't fit. If you clear the pocket with a larger and a smaller tool, the smaller (finish) tool must match the one used for the male part.

Three Inlay Types

1. Straight Inlay (Pocket + Male Plug)

For flat-bottomed inlays where a straight-sided plug sits in a flat-bottomed pocket.

Male (Plug) side:

• Uses a variation of the Profile toolpath that automatically rounds the external corners of the part to allow for the tool radius
• Cuts outside the design vector. There is no Profile Inside or On, and no sharp corners or last pass option, because these do not apply

Female (Pocket) side:

• Uses a variation of the Pocket toolpath, including the option of a larger and a smaller tool to clear the pocket
• Internal corners are rounded based on the tool radius so the male parts fit into them
• A Hole version (a variation of Profile) is available for cutting a cavity that the male shape inlays through

Allowance: The tool radius compensation alone is almost never enough, because the parts would be exactly the same size and would need force or hand work to fit, with no room for a finish. Extra material is cut from the male side, the female side, or both. On Profile-based toolpaths use the Allowance Offset, and on pocket toolpaths use the Pocket Allowance. With letters, the allowance is typically left on the pocket, so the lettering itself is changed as little as possible. Starting values to test on scrap: 0.01" (0.25mm) to 0.02" (0.5mm).

2. Stepped Inlay (Push-Through)

For letters or shapes inserted from the back of a sign, using a step as a shelf that mounts the piece invisibly to the back of the sign.

Settings:

• Step Depth: the vertical height of the step, from the Start Depth down
• Step Width: how far from the edge of the original vector the part is cut out (creating the step)

When inserted from the back, the piece uses the step shelf to seat against the back of the sign material, with the front face flush with the front of the sign.

3. V-Carve Inlay (Automated Toolpath)

The VCarve Inlay toolpath generates the Pocket and Plug toolpaths together in one form, ready for a V-carve inlay piece.

How it works:

• The V-bit carves the pocket (the "socket") into the background material
• A matching V-carve on the plug material creates a mirrored shape that seats into the socket
• Pocket Depth: the maximum depth of the pocket. It may not reach this depth, depending on the vector design and the V-bit angle
• Glue Gap: the distance between the top of the plug and the bottom of the pocket when the two halves are placed together. It must be greater than 0 and less than the Pocket Depth. Common values are 0.001" to 0.01" (0.02 to 0.2mm), depending on the project
• Surface Clearance: affects the gap between the lowest point of the plug and the highest point of the pocket material piece. The higher the value, the less material is left on the plug to remove later. The smaller the value, the closer the two pieces sit and the sturdier the plug is. It must be larger than 0 and lower than the material thickness
• Use Clearance Tools: optional end mill, ball nose or engraving tools to clear large open regions, as in the V-Carve toolpath
• Plug Destination Sheet: the sheet the plug vectors and toolpaths are placed on. On the same sheet they are mirrored from the original position, and on another sheet they are mirrored and moved to the center of that sheet

Critical V-Carve Inlay rule: Use a true V-bit with the correct angle entered in the Tool Database. A tool with a different geometry entered as a V-bit makes the pocket and plug sizes wrong, which gives a poor fit.

Both Pocket and Plug must use the same V-bit. After the original calculation, the Pocket and Plug toolpaths are no longer linked. If you change the V-bit, delete both toolpaths and regenerate a new VCarve Inlay toolpath. If you edit one of them, make the matching change to the other.

Workflow: Classic Straight Inlay

1. Design the inlay shape as vectors (text, artwork)
2. Open the Inlay Toolpath form
3. Select Male type, then choose the end mill
4. Calculate the male toolpath. It rounds the external corners of the plug
5. Switch to the Female (Pocket) type and use the same tool
6. Set the Allowance (a starting point is 0.01" to 0.02")
7. Calculate the pocket toolpath. It rounds the internal corners and applies the allowance
8. Cut the pocket side first (keep the background workpiece on the machine)
9. Cut the plug side from a contrasting wood
10. Apply glue, press the plug into the pocket, clamp and let it cure
11. Plane or sand flush